mach def / post question

[JoE6]

In my pursuit of the "perfect" post for Haas VF5 with 4th axis. I built the mach def, and have modified the post multiple times. one of the things that drives me nuts is it calls out a different WPC for each angle instead of using just G54 and rotating about center. what am I missing here?? is there a simple parameter in the post that needs to be changed, or the machine def?? I havent had much luck trying to locate it. thanks for any input.

[Steve Biehl - Cimquest Inc]

not a simple edit but...

 

- setup a misc integer to flag that you want to lock on first wcs

- save value of first wcs

- use saved wcs if flagged to lock to 1st wcs

[Guest]

Check out the MPMaster available on this site and pull the logic out of that, it's already done and there

 

[Jim Evans from CNC Software]

Mastercam's default WCS value for it's operations is -1 which is the internal flag to mastercam to automatically set new WCS for each change in plane or tool origin. which is why you are getting a new offset for each angle.

 

You can always make a post edit as mentioned above to lock the first WCS, or just use the software the way it is designed and set the correct WCS value in the operation itself.

[Steve Biehl - Cimquest Inc]

Jim,

problem with 'correct' way is that you keep getting the warning dialog of same work offset used for multiple planes. If that could be turned off I opt for the WCS value variable.

[Dan@home]

If you go to settings/machine def manager/edit the control def./(Work system) and set the (Tplane during automatic work offset number creation) to None, the alarm will go away.

[crazy^millman]

Daniel Thanks for that tip. I put it in the Tech tips that is something I did not know either so it has been done to all my Machine/Control Defs.

 

Thank you

Thank you

Thank you

 

Linky:

[Dan@home]

[Roger Peterson]

I don't know that everyone should run out and change this setting. While the work offset error can get annoying it is there for a reason. If you set this to "none" you can get output that would require multiple offsets without giving you any. You can setup a simple toolpath transform using tool origin only and get code that will cut the same part over, and over, and over instead of cutting an array. And you won't get the warning message to alert you that something is awry.

 

 

Now, I've always thought that when this setting was set to "transform toolpaths only" (or whatever it says) you should only get the warning on transform ops, not indexing ops.

 

the lock on first WCS functionality works well, and you setup the post to check the values of the tplane origin and output a warning if they change.

 

Personally I just deal with the warning message, unless a post is stricktly used for rotary work.

 

HTH

[crazy^millman]

Problem I have Roger is I had a 115 operation part on the Integrex and was at one point ready to throw a computer out a window got so tired of this message. I know where and how I want my offsets and I never like anything making offsets for me I want to always make them for myself.

[NeilJ]

Maybe the user should be given more control in the WCS View Manager dialog box? I think the Rotate WCS should have a button in this dialog box and I think you should be able to control this message in the WCS View Manager dialog box as well. Should you be able to attach a WCS to a View Sheet?

[Roger Peterson]

changing this setting will not keep the post from renumber work offsets if workofs$ = -1 or if you use a transform toolpath operation, even if you use match existing work offsets if one is missing it creates a new one. It just keeps the warning message from coming up. I hear you, I don't like the message either, and if you set all your work offsets manually, and check any transform toolpaths you don't have anything to worry about. I just wanted to point out that there are other things to consider and not everyone should change this setting just because.

 

 

regards,

[Dan@home]

If you put a Zero in all of work offsets it will not renumber them and will not recall G54 unless changed, then changed back. Nor will you get this warnning message. For me any way.

 

[ 07-22-2008, 12:57 PM: Message edited by: Daniel@Sierra Cad/Cam ]